What's new
What's new

Long reach small Dia. tools in hard steel

NaRbO

Cast Iron
Joined
Nov 22, 2006
Location
Windsor ON
I've been having some issues with longer reach carbide endmills in hardened h13 tool steel, about 45-48Rc.

The endmills i'm using are mostly OSG and also some Hitachi. We just ran two 3mm OSG WXL ball nose cutters. One had a 12mm reach and the other a 20mm reach. Machine has a max of 15000 rpm. Both cutters were ran at 15000rpm and 51ipm. the 12mm reach ran fine but the 20mm reach tool chipped and left material where it needed to blend. I re ran that tool at 42ipm with a new endmill and it cleaned up but still left a little step and there was a partial chip in one of the flutes after it finished. this is a finishing pass with .003" stock on the mold and a .004" stepdown.

Basically what I do is alter rpm and chipload by a certain percent based on the length to diameter ratio. But i can't seem to find any kind of consistancy with the longer tools. I'm using shrink fit and precision collet holders.

Does anyone have any tips or formulas for these type of situations?

Thanks
 
You usually want to keep the chip load and RPM the same as you would for a normal length cutter, but take less depth of cut and step over. If you slow things down too much the cutter will rub and then you're in trouble. Even if you've got a mile long cutter, it still has to take a chip.
 
Would slowing the rpm down and keeping the same chipload make any difference? I think right now its about a .002 chipload
 
parameters

I've been having some issues with longer reach carbide endmills in hardened h13 tool steel, about 45-48Rc.

The endmills i'm using are mostly OSG and also some Hitachi. We just ran two 3mm OSG WXL ball nose cutters. One had a 12mm reach and the other a 20mm reach. Machine has a max of 15000 rpm. Both cutters were ran at 15000rpm and 51ipm. the 12mm reach ran fine but the 20mm reach tool chipped and left material where it needed to blend. I re ran that tool at 42ipm with a new endmill and it cleaned up but still left a little step and there was a partial chip in one of the flutes after it finished. this is a finishing pass with .003" stock on the mold and a .004" stepdown.
...Basically what I do is alter rpm and chipload by a certain percent based on the length to diameter ratio. But i can't seem to find any kind of consistancy with the longer tools. I'm using shrink fit and precision collet holders.....Does anyone have any tips or formulas for these type of situations?
parameters roughly in inch
carbide end mill .12 diameter
length of flute 0.8
stick out from collet 0.9"
cutting 48 R C scale steel
i get machinability rating of steel roughly 0.3 so
SFPM 340 max
rpm 10,800 max with flood coolant (less without)
feed 5.2 ipm chip thickness 0.0002"
max recommended DOC 0.003"at 100% Width of cut
with a regular end mill. not sure about a ball nose one
.
...... basic rules are 3x the normal stickout length of an end mill and DOC goes down 3x3 or 1/9 AND feed goes down by 1/3 AND a hard material with a low machiniabity rating 0.3 has a lower DOC about 1/3 compared to free machining low carbon steel AND a lower feed too.
.
attached is free Excel spread sheet which does dozens of complex formulas in a millisecond or 2. can also be opened with the free Open Office Calc program. Excel file is in a zip file as thats the only way to attach it.
...... any recommendations it makes need to be verified by your own formulas and calculations. it works fine for my work.
.......formulas get less precise at extreme conditions . i would say a 20mm LOC end mill cutting hardened steel at 48 Rockwell C scale at the extremes
 

Attachments

  • Clipboard01.jpg
    Clipboard01.jpg
    93.9 KB · Views: 585
  • SpeedAndFeedCalculator.zip
    47.5 KB · Views: 95
this endmill doesn't have 20mm flutes, just 20mm of under neck length. its a 6mm shank and only maybe 3mm of flute, the rest of the shank is slightly under 3mm solid carbide and then tapers into the 6mm shank. i've run 1mm by 16mm reach before faster than 5 ipm.

i'm confused because i can rough with this tool and get great life out of it but when i'm finishing its not so good.
 
this endmill doesn't have 20mm flutes, just 20mm of under neck length. its a 6mm shank and only maybe 3mm of flute, the rest of the shank is slightly under 3mm solid carbide and then tapers into the 6mm shank. i've run 1mm by 16mm reach before faster than 5 ipm.

i'm confused because i can rough with this tool and get great life out of it but when i'm finishing its not so good.

You just answered your own question. Try leaving more material to finish...
 
...... basic rules are 3x the normal stickout length of an end mill and DOC goes down 3x3 or 1/9 AND feed goes down by 1/3 AND a hard material with a low machiniabity rating 0.3 has a lower DOC about 1/3 compared to free machining low carbon steel AND a lower feed too.

I can see running at the bottom end on feed, but lower by 1/3rd? That's nuts.
 
i'm confused because i can rough with this tool and get great life out of it but when i'm finishing its not so good.

Do a search on here or google about radial chip thinning. Your finish cut chip thickness is too thin. All this shit matters more as you get into extreme conditions like you have.
 
i've looked at osg and hitachi books, osg gives a .0014 chipload and hitachi gives a .0024 chip load for the same style end mill. I'm aware of chip thinning and i thought these chip loads have already been adjusted for that. So with longer cutters i need to take a bigger cut? feed it faster?
 
I've been having some issues with longer reach carbide endmills in hardened h13 tool steel, about 45-48Rc.

The endmills i'm using are mostly OSG and also some Hitachi. We just ran two 3mm OSG WXL ball nose cutters. One had a 12mm reach and the other a 20mm reach. Machine has a max of 15000 rpm.
Basically what I do is alter rpm and chipload by a certain percent based on the length to diameter ratio. But i can't seem to find any kind of consistancy with the longer tools. I'm using shrink fit and precision collet holders.

Does anyone have any tips or formulas for these type of situations?

Thanks


It is a good thing you are using good quality end mills and holding them well, otherwise it would probably be going a lot worse for you!

Jeff
 
elasticity

I can see running at the bottom end on feed, but lower by 1/3rd? That's nuts.
the rule is stick out 3x more and flexing goes up 3x3x3 or 27 times
.
this is one of those laws of the universe. it does not matter if you do not like the law. thats how objects behave. if you reduce DOC 1/9 and do not reduce feed 1/3 it usually will not break end mill but just vibrate and give a bad finish.
.
chipload charts rarely mention length of end mill sticking out or compensating for harder materials being machined.
.
i have added a line auto compensating for shallow depth ball end mill thinning and this doubled my earlier feed recommendation but i still think too high a feed on a hard steel will give problems. BUT like i said when at extremes like milling hard materials with just the tip of a ball end mill , the Formulas are not very accurate. but it is giving a
feed of 21ipm and not the 42ipm that was tried also
rpm <10800 and not the 15000 rpm that was tried
with a 3mm tip and 6mm shank ball end mill sticking out that far
max DOC recommended went up to 0.039
.
the 3mm dia tip with 6mm shank, in formula their are spots for tool holder length AND a spot for tool holder length effect which i increased from 10 to 200% because the 6mm shank is still a small diameter
........ i never said formulas were perfect, but their the best i got at the moment and that all of my best ideals i can suggest.
 

Attachments

  • SpeedAndFeedCalculator.zip
    48.3 KB · Views: 49
ball end mill at 0.003" DOC

at 0.003" DOC
3mm dia EM
6mm shank
stickout 20mm / 0.8"
hard steel with MR 0.3
.
formula says with chip thinning with ball end mill
<10800 rpm
<41 ipm feed
.
so basically your feed was not that bad but still wouldn't hurt to lower rpm and feed as it maybe it's more the milling hard steel problem
.
probably wouldn't hurt to maybe use some cutting fluid / oil too. partial chip in flutes maybe metal sticking to flutes and oil usually helps
 
the rule is stick out 3x more and flexing goes up 3x3x3 or 27 times
.
this is one of those laws of the universe. it does not matter if you do not like the law. thats how objects behave. if you reduce DOC 1/9 and do not reduce feed 1/3 it usually will not break end mill but just vibrate and give a bad finish.

I wasn't arguing that things don't flex more as they get longer.

If you can lower the feed by 1/3 and still be taking a big enough chip to not rub the end mill to death, than go for it.
 
end mill cutting force calculations

i have been working on a Excel file type calculator version 300 for end mills based on the Horsepower limit of HSS and Carbide tooling based on their diameter and length stick out. Some rules I am using

1) if cutter diameter is cut in 1/2 but length is the same then horsepower limit goes down 0.5*0.5*0.5*0.5 or 0.5^4 power or 1/16

for example
1" dia, 1" shank, 2" flute length end mill taking 3hp if HSS at 150 SFPM
1/2" dia, 1/2" shank, 2" flute can take 3/16 or about 1/5 hp
Carbide can take 3 times more horsepower
.
then calculating if 1018 Steel has Machinability rating of 0.8 which means at 1 horsepower you can mill 0.8 cubic inches per minute. A horsepower is 33,000 ft lbs per minute so for each size (diameter and length) end mill

1) a horsepower rating of end mill can be calculated
2) a metal removal rate can be calculated
3) at a certain chip thickness and SFPM then Feed, Depth of Cut, Width of Cut can be calculated
4) At Feed, DOC. a cutting force can be calculated

so at 3mm Diameter carbide End mill is square end (not ball)
20 mm sticking out
338 SFPM
Machinibility rating 0.3 cubic inch per hp per minute
0.0031" Depth of cut at
Feed 23.5 ipm (chip thickness 0.0011")
10760 rpm
0.0087 cubic inches per min MRR
0.0292 estimated Horsepower
2.8 lbs force (trying to bend cutter)... a odd thing happens as DOC is based on horsepower limit of cutter by slowing down to

200 SFPM that same 0.0292 hp gives
6367 RPM
0.0052" DOC
Feed 13.9 ipm (chip 0.0011" thick)
cutting force 4.8 lbs

because chip thickness is constant at that EM dia and length and using horsepower rating at different SFPM you get different DOC which explains why slowing down RPM and Feed then chatter usually goes down if Depth of Cut does not change
.........i am still checking formulas used but it is a different way of calculating depth of cut. not on what machine has but more what the end mill can take.
maintain SFPM and Slow the Feed and a higher Depth of cut is possible
maintain Chip thickness and Slow SFPM and a higher DOC is possible
......because when you slow rpm speed is converted to a higher torque. higher torque allows higher DOC. to me it is a different way of calculating things. i need to test formulas with different diameters and length and sfpm in the shop to make sure it is accurate.
...... need to double check formulas but it could be useful if you could calculate force on end mill because if you figure a 1000 lbs you obviously need a stronger vise / clamps than if you get only 1 lb of force
 








 
Back
Top